CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

coupling temperature between two solids

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   January 13, 2011, 16:54
Default coupling temperature between two solids
  #1
Senior Member
 
Mirko Vukovic
Join Date: Mar 2009
Posts: 159
Rep Power: 8
mirko is on a distinguished road
Hi,

I am trying to figure out how to solve a temperature conduction problem between two solids using chtMultiRegionFoam. There are no fluids in this problem.

My problem is that I don't know how to couple the temperature across the solid boundaries. I have tried using the solidWallMixedTemperatureCoupled, but that does not work

Code:
        air_to_plate 
        {
         type           solidWallMixedTemperatureCoupled;
         neighbourFieldName T;
         K          K;
         value          293.15;
        }
(disregard the meaning of the `air' label - that is from a solid-fluid version of the problem when air was a fluid. Now I am treating it as solid).

As the problem in the solver that I am using or in the boundary condition?

Thanks,

Mirko

PS - I am attaching the problem files for a simple 2D problem.
Attached Files
File Type: gz two-region-heat-conduction.tar.gz (6.1 KB, 10 views)
mirko is offline   Reply With Quote

Old   January 14, 2011, 05:25
Default coupledMatrix
  #2
mgc
New Member
 
Maria
Join Date: Apr 2009
Posts: 12
Rep Power: 8
mgc is on a distinguished road
Did you try using the "coupledMatrix" instead? (See conjugateHeatFoam)

Marķa
mgc is offline   Reply With Quote

Old   January 14, 2011, 10:55
Default
  #3
Senior Member
 
maddalena's Avatar
 
maddalena
Join Date: Mar 2009
Posts: 436
Rep Power: 12
maddalena is on a distinguished road
Hi Mirko,
Quote:
Originally Posted by mirko View Post
Hi,
I am trying to figure out how to solve a temperature conduction problem between two solids using chtMultiRegionFoam. There are no fluids in this problem.
I run a case like that as well, and the solution is as expected (at least in the temperature distribution). What I have is:
constant/solid1/polymesh/boundary file:
Code:
    solid1_to_solid2
    {
        type            directMappedWall;
        nFaces          10;
        startFace       390;
        sampleMode      nearestPatchFace;
        sampleRegion    solid2;
        samplePatch     solid2_to_solid1;
        offset          (0 0 0);
    }
and 0/solid1/T file:
Code:
    solid1_to_solid2
    {
        type            solidWallMixedTemperatureCoupled;
        value           uniform 300;
        neighbourFieldName T;
        K               K;
    }
That's it! Hope it helps.
mad
maddalena is offline   Reply With Quote

Old   January 14, 2011, 15:10
Default
  #4
Senior Member
 
Mirko Vukovic
Join Date: Mar 2009
Posts: 159
Rep Power: 8
mirko is on a distinguished road
Quote:
Originally Posted by maddalena View Post
Hi Mirko,

I run a case like that as well, and the solution is as expected (at least in the temperature distribution). What I have is:
constant/solid1/polymesh/boundary file:
Code:
    solid1_to_solid2
    {
        type            directMappedWall;
        nFaces          10;
        startFace       390;
        sampleMode      nearestPatchFace;
        sampleRegion    solid2;
        samplePatch     solid2_to_solid1;
        offset          (0 0 0);
    }
and 0/solid1/T file:
Code:
    solid1_to_solid2
    {
        type            solidWallMixedTemperatureCoupled;
        value           uniform 300;
        neighbourFieldName T;
        K               K;
    }
That's it! Hope it helps.
mad
Thank you!

Yep, it helped me track down an incorrect entry in the changeDictionary/dictionaryReplacement/boundary/X_to_Y. I had incorrectly set the sampleRegion as X instead of Y.

I also used the coupling boundary condition compressible::turbulentTemperatureCoupledBaffle (I don't have a clue why that name. Looking at it's .H file the coupling condition looks very general).

Mirko
mirko is offline   Reply With Quote

Old   January 17, 2011, 03:28
Default
  #5
Senior Member
 
maddalena's Avatar
 
maddalena
Join Date: Mar 2009
Posts: 436
Rep Power: 12
maddalena is on a distinguished road
Hi Mirko,
could you post the temperature change in time of some points of your domain and compare them with theoretical time variation? I have some doubts on results I have obtained so far...
Thank you

mad
maddalena is offline   Reply With Quote

Old   January 17, 2011, 10:48
Default link
  #6
Senior Member
 
maddalena's Avatar
 
maddalena
Join Date: Mar 2009
Posts: 436
Rep Power: 12
maddalena is on a distinguished road
posted something on the subject here: http://www.cfd-online.com/Forums/ope...tml#post290772

mad
maddalena is offline   Reply With Quote

Old   January 17, 2011, 12:00
Default
  #7
Senior Member
 
Mirko Vukovic
Join Date: Mar 2009
Posts: 159
Rep Power: 8
mirko is on a distinguished road
Quote:
Originally Posted by maddalena View Post
Hi Mirko,
could you post the temperature change in time of some points of your domain and compare them with theoretical time variation? I have some doubts on results I have obtained so far...
Thank you

mad
I want to cleanup my setup & generate some benchmark cases. I will then post my setup and results.

Mirko
mirko is offline   Reply With Quote

Old   January 19, 2011, 18:58
Default
  #8
Senior Member
 
Mirko Vukovic
Join Date: Mar 2009
Posts: 159
Rep Power: 8
mirko is on a distinguished road
Quote:
Originally Posted by maddalena View Post
Hi Mirko,
could you post the temperature change in time of some points of your domain and compare them with theoretical time variation? I have some doubts on results I have obtained so far...
Thank you

mad
Hi Maddalena,

(got busy with paperwork)

Unfortunately, I managed to break my two-region problem and loose the temperature connectivity across the interface.

FWIW I am attaching two archives:
  1. The broken two region problem that illustrates my predicament
  2. A simple 1D thermal conduction problem that I wanted to use for benchmarking of the above model. This is a very unphysical one: temperatures between 0 & 1. This simple model is working.
Thanks,

Mirko
mirko is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Calculation of the Governing Equations Mihail CFX 7 September 7, 2014 06:27
Fluent Ansys temperature coupling tensun Fluent UDF and Scheme Programming 0 November 14, 2010 06:30
high temperature in a coupling simulation sheintz STAR-CCM+ 3 September 30, 2010 13:56
How to set Temperature as heat source in Solids shahpar73 CFX 2 August 20, 2009 18:51
Coupling CFX4 with a solids code Brett Towler CFX 1 September 20, 2000 20:09


All times are GMT -4. The time now is 21:03.